I have a question regarding differential signals/routing:
<> If you have upto 16 differential line pairs and you have to go through
a connector to terminate the differential signals on a daughter card, what
is the best signal to gnd ratio and pattern one should consider using?
In this case the connector is a high density pin connector. If the
differential impedance (of the line traces) is 100 ohms do I need a special
Ground pattern, as the signals go through the connector, to maintain the
differential impedance close to 100 ohms?

I've recently started my first high-speed digital
design and have found your book to be extremely
valuable.

I have a question regarding the routing of
differential pairs such as ECL or LVDS. It has
been suggested that routing differential pairs as
overlapping signal traces on adjacent layers is
superior to routing them as adjacent traces on the
same layer.

I have been unable to find any literature that
characterizes this geometry and was wondering if
you could recommend a reference or had any comments
on the subject.

Thank you,
Clint Lieser

*--------------(REPLY FROM DR. JOHNSON)--------------*

Thanks for your interest in High-Speed Digital
Design.

I don't have any references to give you but I do
have a couple of comments.

First, either structure can work.

Second, with either structure it's not particularly
important that the lines be coupled tightly
together. In fact, you couldn't achieve very tight
coupling even if you tried. The coupling ratios
(effectively the common-mode rejection of the
structure) for typical differential lines on PCB's
are only in the 20-50% range.

In contrast, for a well-balanced differential
twisted pair, the coupling is 99.9%. That is, if I
transmit a signal down one wire of a twisted pair,
with the other wire grounded, at the far end I will
receive two signals, each of half size, and having
opposite polarities. This is the property called
"good common-mode rejection".

To get good common-mode rejection what you need is
a crosstalk coefficient of about 99.9 percent.
Differential traces on a PCB won't do that.
Fortunately, we don't need this property for PCB
applications.

Here's a list of the reasons we normally use
differential pairs on a PCB:

(1) To match to an external, balanced differential
transmission medium (some kind of cabling). For
this purpose, the inter-trace coupling is
irrelevant. Two independent, 50-ohm traces can
couple a perfectly fine signal into a 100-ohm
differential transmission line. What we want in
this application is to make sure that the signal is
generated in a purely differential manner (no
common-mode components that would radiate off the
cable). Furthermore, we want to make sure that the
two PCB traces have equal impedances to ground
(that is, they need to be symmetrical, but not
necessarily close together).

(2) To defeat ground bounce. A differential signal
naturally comes with its own built-in reference
voltage. The receiver of a differential signal
therefore does not need to rely on its own built-in
reference, which could be corrupted by ground
bounce voltages internal to the receiving device.
For this purpose, we need only supply the receiver
with two antipodal signals, with equal delays from
the driver. There is no requirement here for
particularly close coupling.

(3) To reduce EMI. The radiation from one trace of
a differential pair is cancelled by the radiation
from the adjacent trace, resulting in a marked
reduction in emissions. The cancellation is
proportional to the ratio S/D where S is the trace
separation, and D is the distance to the receiving
antenna. If we are talking about FCC class B
measurements, which are taken at a distance of 3m
(117 inches), then a 1-inch separation would yield
a 40-db improvement in EMI (a whopping big
improvement). A 0.1 inch separation should yield 60-
db. Both of these numbers are probably better than
the common-mode balance between the two outputs
that created the differential signal in the first
place. That is, with a separation of 0.1 inch, we
have balanced the signal as well as could be done
given the imperfections in the source, and
certainly at the 0.1-inch separation level we have
probably knocked down emissions to a level far
below FCC limits. For EMI purposes, a differential
trace spacing of 0.1 inches is close enough to do
the trick. We need not struggle to place the
traces any closer than that as far as our EMI
requirements are concerned.

(4) To reduce local crosstalk. Differential traces
on a PCB do a poor job of this. As mentioned
above, signal cancellation is a function of the
ratio of the trace separation, S, to the distance,
D, to the receiving antenna. For local interference
(which can be very, very close), you don't get much
cancellation. Whether you use differential
signaling or not, the best way to improve local PCB
crosstalk is to move the effected traces further
away. Assuming you have solid power and ground
planes, crosstalk between aggressor and victim
traces falls off as the SQUARE of increasing
distance. Doubling the distance cuts crosstalk to
one-fourth. Cramming the two traces of a
differential pair closer together helps reduce
crosstalk, but you don't get the big SQUARED
benefit you get from generally increasing the
separation between aggressor and victim.

(5) To improve routability. Differential traces
CAN be pushed really, really close together, which,
if you have oodles of them, can save board area.
In my opinion, the desire to save board area is the
only motivation for using an unusually close
spacing. Remember that once you have committed to
the use of tightly packed, differential traces, you
will forever be hampered by two effects: (a) you
will need to compute a new trace width to
compensate for the fact that the differential
impedance goes down for closely spaced signals, and
(b) once the signals are paired, they CANNOT be
separated, or else you will mess up their impedance
(unless you go back to fatter widths).

This second effect imposes a routing penalty on the
side-by-side approach. It's hard to get these
traces to go around obstacles without the ability
to temporarily separate. The over/under format
works better for long-distance complicated routing.

What do I do? Unless absolutely pressed for space,
I'll choose the side-by-side format. I will set
the trace separation at about 4H (which yields only
6% crosstalk, or only about 6% effect on
impedance). I will instruct my layout person to
keep these traces generally near each other, but
permit them to separate from time to time as needed
to go around obstacles. I will also insist that
they be equal in length.

If you use the over/under format you should know
that there is a subtle asymmetry built into this
configuration. The distance from the top surface of
the board down to the bottom trace is greater than
for the top trace, and also any return currents
associated with the bottom ground plane have to
find nearby vias to provide pathways back to the
top surface. The net effect is that the bottom
trace has some extra delay built in at the
endpoints. To minimize this problem, make sure you
put a number of ground vias near the point where
the signals originate.

I've heard reports of additional bottom trace
delays in the range of 100 ps (in that particular
design, at each end of the line, the return current
had to divert about 0.16 inch out of its way, and
then come back, giving a total additional delay of
0.14*2*(180 ps/inch) at each end). If 100 ps
matters to you, then either put the vias closer, or
don't use the over/under format.

Best regards,
Dr. Howard Johnson

*----------------------------------------------------*

Comments welcome! hsdd@signalintegrity.com

To unsubscribe from this list: send an email to
hsdd@sigcon.com with "unsubscribe" in the subject
line. To subscribe to this list: send an email to
hsdd@sigcon.com with "subscribe" in the subject
line. Include your name and email address in the
body of the message. (NOTE: If you received this
message, you do not need to re-subscribe.)

**** To unsubscribe from si-list: send e-mail to majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****